WORKBENCH - How useful are bolt loadings?

[Shockdesigner331]

Hello everyone. I am currently working on a few mounting brackets. I designed the brackets using SolidWorks and decided to import them into Workbench for analysis. I'm new to ANSYS but Workbench seems fairly easy to learn. I decided to add a few bolts to the mounting brackets and apply a bolt preload to them (100 kips). I modeled only the portion of the nut that was not fastened by the nut, one end is attached to the bracket the other end is hanging in space. My questions are:

1)Does the bolt load apply a fixed restraint to one end? It appears that it does. Can I assume that the "working load" calculated by ANSYS is the reaction force at the bolt?

2.) How accurate is this solution when compared to a classic ANSYS analysis?

Is there another way to go about finding the bolt loads? I thought about using fixed restraints at the hole locations but this wouldn't be accurate because of bolt elongation.

Any Tips or comments would be greatly appreciated. Thanks.

-Mike

 

[Drej]

> 1)Does the bolt load apply a fixed restraint to one end? It appears that it does. Can I assume that the "working load" calculated by ANSYS is the reaction force at the bolt?

The bolt load is achieved in ANSYS using CEs (constraint equations) at the cut portion, then creating a reference node which the load is applied to (the creation of the CEs is performed using PRET179 elements, and is done internally for you in Workbench, as is the creation of the reference node - but not in ANSYS). All restraints need to be added by the user. If you want to remain in control of your analysis, I would add these constraints in. The reaction load is, as you've stated, the preload seen by the bolt.

> 2.) How accurate is this solution when compared to a classic ANSYS analysis?

'Tis exactly the same, Workbench just automates some of the steps to make it easier for the user.

> Is there another way to go about finding the bolt loads? I thought about using fixed restraints at the hole locations but this wouldn't be accurate because of bolt elongation

There are many ways using FE, but within Workbench you're restricted to this much pretty much. The (harder/more work) alternative is to model the bolt as a line element (i.e. a beam or link element) and add initial compressive strain to the element to provide the preload. You would then need to connect the link/beam to the outer edges/nodes of the component using a "spider" of other beams, then write constraint equations to tie the DOF together at the interface between the solids/beams. Not straightforward, ans certainly not in Workbench (if you have an ANSYS licence then it's considerably easier to do *some* steps, but it's still a bit of work). Your best bet in my opinion is to use the method you've outlined (using the bolt preload feature) but just make sure it's constrained correctly and that the correct contact is being simulated at the interfaces (bonded contact is usually sufficient).

Cheers,

-- drej --